Application of ‘Circular Pattern’ tool-Autodesk Inventor 2013 (with caption and audio narration)
Serial No. 197 Application of ‘Circular Pattern’ tool-Autodesk Inventor 2013 (with caption and audio narration) Transcription of Video This is the model of Twist Drill that is created by us earlier. A full-fledged video related to this can be found on our You Tube Channel. Here from the Browser Bar you can check the history of its modelling. A lot of 2D sketches, Extrude, Coil features, Work features and Circular Pattern were utilized to create this model. In this video we will describe about the Circular Pattern Tool that was used three times in its modelling. Watch the video to understand how the tool works. Circular Pattern tool duplicates one or more features and arrange the resulting occurrences by a specific count and spacing in a circular path. This tool is available on Pattern Panel of Model Tab. First Circular Pattern Applied in the modeling of Twist Drill After activating the Circular Pattern tool the Coil1 and Extrude2 are being selected as feature for the duplication. Z axis of the model has been selected as axis of revolution. The number of occurrences in the pattern is 2. Degree of rotation is 180. After clicking the ok button the result is in front of you. A duplicate feature is created easily. Watch the past and current position of the model by suppressing and un-supressing the feature. Second Circular Pattern Applied in the modeling of Twist Drill. This time Extrude4 is selected as feature and the Rotation of Axis is same that is the Z axis of the model. The Occurrence count will be 2 and the Occurrence angle180 degree. After clicking the ok button the duplicate feature is created. Third Circular Pattern Applied in the modeling of Twist Drill. This time two Coil features are selected for the duplication. All the other specifications of the Circular pattern will be the same as previous ones. The final result is visible in the design window.
Application of ‘Sweep’ tool and ‘Shell’ tool-Autodesk Inventor 2013 (with caption and audio narration)
Serial No. 196 Application of ‘Sweep’ tool and ‘Shell’ tool-Autodesk Inventor 2013 (with caption and audio narration) In this exercise we will create a new part, related to our previously created full-fledged model ‘Elbow’. In this part file we will create some 2D Sketches, work planes, sweep & shell features. Click the following link to get the model file: – http://bit.ly/2nPe9Wf Transcription of Video Create a New Standard (in).ipt file. Create a 2D Sketch on the XY Plane. Draw a line of length 1.1875 inch, coincident with the auto projected part origin and parallel to X axis. Right click in the graphics window and select ‘Create Line’ tool. Click the green point in the graphics window as start point of the line. And enter the value 1.1875 inch. Right click in the graphics window and click OK to finish the command. Create another line of length 1.1875 inch, parallel to Y axis and coincident with the origin. Select these two lines and change the colour to White. On the Ribbon click ‘Fillet’ icon on the Draw panel of Sketch tab. 2D Fillet dialogue box is visible in the graphics window. Enter the value 0.625 inch in the 2D fillet dialogue box. And select these two lines in the graphics window to apply the fillet. Right click in the graphics window and click OK to exit the command. Finish the 2D Sketch. On the Ribbon click ‘Plane’ icon on the Work Features panel of 3D Model tab. Click one of the end points of the line and select this line in the graphics window. Work Plane has been created, perpendicular to this line. Create a new sketch on this Work Plane. Draw a Circle of diameter 1 inch on the end point of the line. Finish the 2D Sketch. Activate the ‘Sweep’ tool from Create panel of 3D Model tab. Sweep dialog box is visible in the graphics window. Since there is only single closed profile, the profile drawn on sketch 2 is selected automatically. The path selection button is active in the Sweep dialogue box. Select the ‘Sketch1’ in the graphics window as sweep path. Click OK to execute the Sweep feature. Change the model colour to ‘Flaked Reflective – Beige’. Save the Part file with the name ‘Elbow’. On the Ribbon click ‘Shell’ tool icon on the Modify panel of 3D Model tab. Shell dialog box is visible in the graphics window. ‘Remove Faces’ selection button is activated by default. Select both blue faces of the Elbow. Enter the value 0.125 inch in the ‘Thickness’ field. Click OK to apply the Shell feature.
